[a7medalsalmi]

Hello,

I have been trying to simulate an axisymmetric CD nozzle with an atmospheric domain to observe the flow after the exit area. I am trying to replicate the problem shown in: https://pp.bme.hu/tr/article/view/11490/7907 with the same Boundary Conditions (Pressure Inlet, Pressure Outlet, Farfield Pressure, Free slip wall, and axis).

Although, I have faced multiple warnings in console when running the calculations such as:
*.temperature limited to 5.000000e+03
*.absolute pressure limited to 5.000000e+10
*.time step reduced in 133 cells due to excessive temperature change
*.turbulent viscosity limited to viscosity ratio of 1.000000e+05

I am not sure what exactly is the problem as I tried to change the Boundary conditions multiple times to investigate what would work. I am pretty sure my mesh is accurate as well with skewness below 0.3, with clustered cells near the nozzle wall which is the area of interest.

I would really appreciate if someone could point me in the right direction.

[AlexanderZ]

there are several tutorials regarding this simulation on youtube
first recommendation (besides mesh quality) patch pressure in chamber,
start with small pressure, converge, increase pressure, and so on

[vinerm]

What I would doubt are not the boundary conditions or the mesh rather the material properties and operating conditions. Could you share a snapshot of material and operating conditions panel?

Assuming that everything is setup correctly, try fmg-initialization. This works like a test for such cases. If the fmg-initialization is successful, then the case is setup properly, else you need to modify something.

[a7medalsalmi]

Hello Alexanderz I appreciate the quick reply.

I have been through the tutorials online, however, most of these tutorials simulate the CD Nozzle without an atmospheric domain. I could get the simulation to converge if I replicate their method, but I am also interested in simulating the flow after it exits the nozzle in an atmospheric layer.

I am not sure exactly what I am doing wrong as I have followed every step mentioned in the paper I mentioned previously, and I also tried using different Boundary conditions such as the mass inlet flow rate to get the calculations to converge but unfortunately, nothing worked thus far.

[a7medalsalmi]

The material properties I used: Ideal Gas, Sutherland viscosity. The operating conditions I changed to 0.

I'm still somewhat a beginner in CFD, but I'll try and learn how fmg-initialization would work. Thank you for your quick reply.

Hopefully I'll figure out what I am doing wrong! Would it be possible if I uploaded the files so you could take a look at my simulation? Currently using Ansys version 19.2.

[vinerm]

If operating pressure and operating density, both are set to 0 values, then you have to ensure that at the inlet and outlet boundaries, absolute pressure values are used. So, even if you give mass flow inlet at the inlet you have to ensure some positive value in Supersonic/Initial Gauge Pressure. Similarly, outlet should have 101325 Pa.

For fmg initialization, you need to use commands

solve init fmg-init

[a7medalsalmi]

I haven't thought about operating density tbh. I am not sure how to change that but I'll figure it out. I'll try fmg-initialization and I'll get back to you. Thanks!

[vinerm]

Operating conditions panel has both, operating pressure and operating density. Both should be set to 0

[AlexanderZ]

it took 10 sec to find this link
https://www.youtube.com/watch?v=oY_3_c0rDiw

everything had been done already, search

[a7medalsalmi]

Yes and I told you, I have been through these videos. I already saw the video that you linked, and I tried to replicate everything he's done as well but to no avail. I still get divergence when running calculations. I am not sure what I am doing wrong.

[vinerm]

Was it successful with the fmg-initialization?

[a7medalsalmi]

Hey vinerm.

Unfortunately, it was not successful. The solution was diverging once again. Below was the output I got after the command:

" solve init fmg-init
Enable FMG initialization? [no] yes

Creating multigrid levels...
Grid Level 0: 97750 cells, 196311 faces, 98562 nodes; 2 clusters
Grid Level 1: 24487 cells, 98674 faces, 98562 nodes; 2 clusters
Grid Level 1: 24487 cells, 49810 faces, 0 nodes
Grid Level 2: 6216 cells, 50159 faces, 98562 nodes; 2 clusters
Grid Level 2: 6216 cells, 13175 faces, 0 nodes
Grid Level 3: 1568 cells, 25641 faces, 98562 nodes; 2 clusters
Grid Level 3: 1568 cells, 3807 faces, 0 nodes
Grid Level 4: 413 cells, 13619 faces, 98562 nodes; 2 clusters
Grid Level 4: 413 cells, 1467 faces, 0 nodes
Grid Level 5: 106 cells, 7363 faces, 98562 nodes; 2 clusters
Grid Level 5: 106 cells, 836 faces, 0 nodes
Done.

absolute pressure limited to 5.000000e+10 in 4 cells on zone 3

temperature limited to 5.000000e+03 in 27 cells on zone 3


FMG: Converge FAS on level 5


FMG: Converge FAS on level 4


FMG: Converge FAS on level 3


FMG: Converge FAS on level 2


FMG: Converge FAS on level 1
0.
Reversed flow in 150 faces on pressure-inlet 6.

reversed flow in 3 faces on pressure-outlet 10.

time step reduced in 536 cells due to excessive temperature change

absolute pressure limited to 1.000000e+00 in 2 cells on zone 3

absolute pressure limited to 5.000000e+10 in 869 cells on zone 3

temperature limited to 5.000000e+03 in 2514 cells on zone 3
->1.->2.->3.->4.->5.<<<<<

turbulent viscosity limited to viscosity ratio of 1.000000e+06 in 117 cells

turbulent viscosity limited to viscosity ratio of 1.000000e+06 in 116 cells"

[vinerm]

Well, that explains it. As stated, if the fmg-initialization is not successful, there is something wrong with the setup. Could you share snapshots of material properties, boundary conditions, and operating conditions? Solver settings and mesh quality would also be useful.

[a7medalsalmi]

Sure no problem.

solver settings: https://postimg.cc/KR5f78jN
Boundary conditions: https://postimg.cc/ThfWVqDz
material properties: https://postimg.cc/nsfq68Xz
operating conditions: https://postimg.cc/JyHdQC9z
mesh: https://postimg.cc/RWk2y01H (skewness below 0.4)
https://postimg.cc/9DLBKm6B

Thank you!

[vinerm]

Rest appear to be good but there are two things

1. By boundary conditions, I mean the conditions applied at the boundary; images from Fluent. And you seem to have a mix of the conditions. Such as far field and free-slip. Furthermore, you have far-field attached to the wall. This is not allowed and supposedly the reason for fmg-initialization failure. Best would be to make all of these pressure outlet, i.e., C, D, and E, all should be pressure outlet.

2. Secondly, what is the Mach number for your case? If it is less than 2, I'd recommend using pressure-based solver with pseudo-transient coupled solver.

[a7medalsalmi]

Pressure inlet (Temperature=400K): https://postimg.cc/BtrCDw3J
Pressure outlet (Temperature=300K): https://postimg.cc/ygzZx29G

I also attached the initial values from inlet: https://postimg.cc/2bF2SQq4

I tried changing the boundary conditions as you suggested. A divergence is still occurring when running the calculations. This is what was prompted in the console:

"solve init fmg-init
Enable FMG initialization? [no] yes

Creating multigrid levels...
Grid Level 0: 97750 cells, 196311 faces, 98562 nodes; 2 clusters
Grid Level 1: 24487 cells, 98674 faces, 98562 nodes; 2 clusters
Grid Level 1: 24487 cells, 49810 faces, 0 nodes
Grid Level 2: 6216 cells, 50159 faces, 98562 nodes; 2 clusters
Grid Level 2: 6216 cells, 13175 faces, 0 nodes
Grid Level 3: 1568 cells, 25641 faces, 98562 nodes; 2 clusters
Grid Level 3: 1568 cells, 3807 faces, 0 nodes
Grid Level 4: 413 cells, 13619 faces, 98562 nodes; 2 clusters
Grid Level 4: 413 cells, 1467 faces, 0 nodes
Grid Level 5: 106 cells, 7363 faces, 98562 nodes; 2 clusters
Grid Level 5: 106 cells, 836 faces, 0 nodes
Done.


FMG: Converge FAS on level 5


FMG: Converge FAS on level 4


FMG: Converge FAS on level 3


FMG: Converge FAS on level 2


FMG: Converge FAS on level 1
0.
reversed flow in 28 faces on pressure-outlet 8.

reversed flow in 26 faces on pressure-outlet 9.

reversed flow in 14 faces on pressure-outlet 10.

time step reduced in 16 cells due to excessive temperature change

absolute pressure limited to 1.000000e+00 in 1 cells on zone 3
->1.->2.->3.->4.->5.<<<<<"

[a7medalsalmi]

The mach number for my problem would around 4.2. Thus, a density-based solver seems more appropriate.

[vinerm]

With pressure outlet, fmg initialization seems to be better. There is only one cell that has temperature limit applied. To improve this, you can disable secondary temperature gradients using following command

(rpsetvar 'temperature/secondary-gradients? #f)

One more thing, is it Implicit method you are using or Explicit? Usually, such high Mach number simulations require proper solution steering.

[AlexanderZ]

increase pressure in chamber gradually, start with low value
when you are talking about Mach number do you mean external flow? If so, increase speed of external flow gradully too

[a7medalsalmi]

Alright, for those of you who are approaching this CFD problem and are undergoing similar issues, I managed to solve it by applying a combination of solutions:

1. Make sure that you adhere to good meshing habits, even though your mesh might be very fine and clustered along the nozzle wall, the cells shouldn't jump in size suddenly so be careful when using the hard biased cells option. Also, read on the y plus value and make sure for this specific problem to have the y plus be less than 1 to get accurate results regarding the shock placement along the nozzle wall.
2. Specify the hydraulic diameter as the nozzle inlet to ensure an accurate representation of the inflow duct of the experimental equipment.
3. Try a range of courant numbers starting from the default number of 5 and lowering it up to 1 and less and observe which courant number provides the best convergence.
4. Try a Spalart All-maras turbulence model first as it is a simpler one equation model which takes less time for the solution to converge, if you are interested in capturing the flow separation accurately you can try the k-w SST model later on.